text symbol line weight (line thickness) & making different size formats

[Inoram]

Hello,

In Creo2 I am setting up my format and trying to make everything look as nice as possible. So I picked a font and setup all the text thickness so everything looks nice in drawing mode and in PDF. The only thing left that I cannot figure out is how to make the text symbol elements look good. Currently they are thin lines in drawing mode but in a PDF they are fat.

Is there a setting I missed to set text symbol line weight?

My other issue is, now that I spent the time to make a nice looking format, I have not yet been able to figure out how to easily duplicate it to another size.

This one I just started working on this morning, maybe there is something simple I am missing.

thank you

Matt

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[TomD.inPDX]

You can save the tables and you can save-as the formats. Generally it is a very manual process.

The actual symbols should take on your text thickness attributes but the surrounding boxes take on the lettering pen widths. If these require more thickness, I suggest using pen tables for plotting. If the text is too small on the formats, it could become a bit blotchy.

I have my text line thickness set to .012 and plot with the default pen tables for the witness/dimension lines. I also use one of the ISO fonts as a default font. These come out very readable in PDF even if D-size is printed on A-size... with reading glasses, of course.

[Inoram]

Thank you for the input. The text thickness setting changes it, interestingly though, the format is not pulling the text thickness setting from the prodetail.dtl like a drawing is. So when editing the format it looks odd, but then using it in a drawing it comes out correct.

I am using the TTF CG Triumvirate at the moment. It seemed like a clean, readable font when I looked through them. And so far it looks good on what I have created.

But currently, I have a B size format that I think is done and I need a to make a D size version. So yes, I did a save-as, but when I load the copy I have not yet been able to figure out how to make it a D.I hope I am just missing a setting somewhere that I can adjust.

[TomD.inPDX]

Ah... yes. Now I remember. That is why I was saving tables so I could use them in new formats. I do this so rarely I forget the limitations. I think the only shortcut you can use is to export and import the geometry as DXF in the new file.

I remember something about converting drawings into formats... probably as drawing templates. Hopefully someone can weigh in here. I know the discussion has come up before.

And yes, TrueType fonts ignore "thickness" settings at least on the screen. You have to assign a default thickness to the symbols to try to match the TTF lineweights. Are you saying that the TTF is plotting by adding the default thickness?

[Inoram]

I went ahead and saved out the tables, started a new D size format and loaded the tables back in, this worked fine, it saved the text style data (copy and paste would not). And with the grid on and snaps on it was easy to line everything back up. I was trying to avoid import/export. My previous formats were created this way and I was attempting to clean everything up by going all native.

The TTF seems to be printing and PDFing fine so far. The text symbols were the only elements that appeared odd, and I think that was mostly because I did not realize the text thickness setting was controlling them.

[BrianMartin]

Hi Matt...

The number of odd little idiosyncrasies and weird trivial bits of knowledge you need to know to effectively put together new formats is huge. I typically start with designing the title block grid for a D-sized sheet. I then use that same grid for the other sizes, too. If you really want them to look nice, you have to partition the table into a fairly tiny little grid and then merge cells together to make larger and larger cells.

On our formats we have all sorts of data, little checkboxes, and other whizbang "kewl" things that took forever to set up. There are a whole host of important, yet overlooked pieces to the puzzle:

• Make sure to set up the Zones of your format so you can take advantage of the automatic zone location features of Creo. This helps with the creation of zone locator blocks and notes.
• Pay careful attention to the parameters you want on your drawing. Do you want to spend time filling in a million little boxes each time you start a new drawing? If not, pay attention to parameters.
  • Many people think the only way to drive a format to automatically fill in information is to put all of their parameters in their models. This is not true.
  • Put parameters that make sense for the model in the model. Put parameters that make sense only for the drawing in the drawing.
• The format is important... but not nearly as important as your templates. Templates are to formats what cars are to bicycles. If you're trying to get somewhere fast, you wouldn't hop on a bicycle (unless it's a very short distance). Same thing for templates... you need them... they make your life much easier and help enforce standards.Formats cannot contain symbols, notes, pre-loaded views and other helpful information... templates can.

To solve your problem with the printing of symbols, you definitely want to take advantage of a pen table file. Somewhere on PTC Community I put together a very long post about how to use these (for Wildfire 5). I don't believe they've changed for Creo. Take a look at this thread and see if it helps.

If you need any other help, have additional questions, or just need some guidance, let us know.

Thanks!

-Brian

[Inoram]

Brian,

Thanks for the input. In past I have not used models to drive parameters (except model name), and I have used a bunch of the auto ones (scale, date, etc). and then the ones that vary I type in when creating the drawing (the windows that pop up and you fill out the info). But I only fill out about 5 things. I have always assumed and could be wrong that I could drive parameters with Excel, but I have never tried it.

As far as drawings templates, please tell me how I could use them. I have actually never used them, the only thing I could think of putting in the template is some notes I commonly use, but maybe that's not the right spot for them either (as I would be deleting out the ones I didn't need).

thanks!

Matt

[BrianMartin]

Hi Matt...

You actually cannot fill out the parameters via Excel (at least not currently). You can set things up so you don't have to answer those questions each time you open a new drawing, though. You can fill them out later by simply double-clicking the blank fields and filling in the data if you're using a template.

It's perfectly fine to add your standard notes to a template. If you have to remove some notes, I find it's easier to remove than to add/load new ones. Other things you might add to a template are standard symbols that you often use. For example, do you add finish symbols, weld notes, or flag notes often? If so, you're probably used to loading them from the symbols palette. Once they've been loaded once, you can find them easily... but the first time you used it, you had to go hunt for it and load it into the drawing. With a template you can pre-load the symbols.

Some people see a template ONE thing. For example, they think that a template has to be a basic, blank page that can be used for any drawing. But you can have dozens of templates for specialized uses.

Let's say you do lots of drawings of cut pieces of tubing. You make many of these drawings and they're all very, very similar. They have the same notes, BOMs, symbols, and views. You can turn any one of those drawings into a template. That way the next time you need to make a similar drawing, most of the work is already done.

You could have templates for assemblies, weldments, piece parts... or you could have specific templates for plates, machined items, cast parts, plastic items, etc. There's no limit to the number of templates you can have. A template is just a drawing that's been pre-formatted. Templates have the .DRW extension... they are literally JUST a drawing. You can add some special icons and tools to them to automatically create drawing views, etc... but mostly they're just a drawing.

Take a look at the help files for creating a template. Once you've read through it, ask any specific questions you have. There's a bit too much to give you a tutorial in a message such as this but I can help guide you after you've read up on the basics.

Thanks and good luck!

-Brian

[Inoram]

Brian,

Again, thanks for the information. I am mostly doing mold design. So I am doing a lot of custom pieces. I need to read through the PTC stuff you suggested.

But here's a simple question, how do you un-activate a part after working on it in assembly mode? Previously regen did this, but I can see how people did not like constantly re-activating the part they were working (or accidently adding a feature to the assembly versus the part, which I did once in awhile).

Matt

[TomD.inPDX]

Right click on the assembly in the model tree and activate the assembly.

[Inoram]

Thanks again!

I am still getting used to the differences form WF3. Actually the difference overall seems fairly minimal.

Is there any way to turn of Xhatch in a 2D section?

thanks!

[Inoram]

Nevermind! I found it. yes, still getting used to the changes. All in all some nice tweaks to go a little faster, but some things still need improvement.

[ptc-255508]

config.pro :

pdf_use_pentable yes

pen_table_file C:\..\pdf_pen_table.pnt

Just check in your pdf export settings that Use pentable is ticked

*.pnt is a text file :

!pen 1 = geometry (white)

!pen 2 = letter (yellow)

!pen 3 = hidden (gray)

!pen 4 = highlight primary (dark red/red/orange)

!pen 5 = sheet metal(dark green)

!pen 6 = sketched curve (blue)

!pen 7 = highlight secondary (dark gray)

!pen 8 = highlight edge (green)

!

pen 1 thickness .005 in

pen 2 thickness .005 in

pen 3 thickness .002 in

pen 4 thickness .015 in

pen 5 thickness .008 in

pen 6 thickness .005 in

pen 7 thickness .010 in

pen 8 thickness .005 in